Getting best surface finish OD turning 6061 AL?

[SRT Mike]

I am turning 6061 Aluminum, to a finished diameter of around 2.25". The part is around 3" long and it is an arc (it ends up being something of an egg shape).

Any recommendation on how to get the absolute best surface finish? Machine is very big and rigid - Okuma LC40 and has a max spindle speed of 2500RPM.

What type of insert should I use - what geometry and (if applicable) what coating on the toolbit insert to get the best finish? What about the feed and speed?

The parts are going to get anodized later so if I can get a ready-to-anodize finish it would be perfect!

[harryn]

Hi , My machining experience is limited, but one thing I have seen with Al - it is much easier to get a nice finish on 7000 series than 6000 series Al. It can also be anodized similarly, but you end up with a harder, stronger, tougher part.

[tobyaxis]

Originally Posted by SRT Mike I am turning 6061 Aluminum, to a finished diameter of around 2.25". The part is around 3" long and it is an arc (it ends up being something of an egg shape). Any recommendation on how to get the absolute best surface finish? Machine is very big and rigid - Okuma LC40 and has a max spindle speed of 2500RPM. What type of insert should I use - what geometry and (if applicable) what coating on the toolbit insert to get the best finish? What about the feed and speed? The parts are going to get anodized later so if I can get a ready-to-anodize finish it would be perfect!

Lower your RMP to about 1200. Then Feed at .002 IPM with a .008 Tool Nose Radius. You will have to play with this to get the best finish while maintaining good production. This will give you around a 20 Micro Finish.

The Egging is being caused by Vibration in the Spindle which was more than likely hit a few times. Or the Bearings might be a little sloppy from many hours of use.

Also if this Shaft is long and you are using a Live center make sure it isn't a cheap one.

The only way I have found to take the Slop out of a Spindle is to reduce the RPM and try to maintain a productive run off of parts.

Inserts, try Sandvik. The Carbide Grade should be a C1 with a Positive Rake and a good Coating like TiALN. This coating keeps material from welding itself to the insert land at the Nose Radius. You will have to know the Size Insert for your tool holder too.

My best guess is that your machine has 1 inch tool shanks with CNMG, DNMG, or VNMG style Inserts. If so you will be looking for CNMG430.1 ANSI Designations for the .008 TNR.

Oh, it is wise to use a depth of cut that is slightly more than the Nose Radius. so be sure to leave enough for finish.

Cheers!!

[SRT Mike]

Originally Posted by tobyaxis Lower your RMP to about 1200. Then Feed at .002 IPM with a .008 Tool Nose Radius. You will have to play with this to get the best finish while maintaining good production. This will give you around a 20 Micro Finish. The Egging is being caused by Vibration in the Spindle which was more than likely hit a few times. Or the Bearings might be a little sloppy from many hours of use. Also if this Shaft is long and you are using a Live center make sure it isn't a cheap one. The only way I have found to take the Slop out of a Spindle is to reduce the RPM and try to maintain a productive run off of parts. Inserts, try Sandvik. The Carbide Grade should be a C1 with a Positive Rake and a good Coating like TiALN. This coating keeps material from welding itself to the insert land at the Nose Radius. You will have to know the Size Insert for your tool holder too. My best guess is that your machine has 1 inch tool shanks with CNMG, DNMG, or VNMG style Inserts. If so you will be looking for CNMG430.1 ANSI Designations for the .008 TNR. Oh, it is wise to use a depth of cut that is slightly more than the Nose Radius. so be sure to leave enough for finish. Cheers!!

Thanks for the info Toby, I realized later I should have posted this in general machining discussion, not machine tools

The egg shape I mention is actually how the part is supposed to look - it's basically a bullet type shape - if you look at it in cross section, it would be a parabola (so it's like half an egg). I need to start with about 2.5" bar stock and turn this profile into the part. I also need to bore out the inside and then with the live tooling mill a flat on the outside and then drill the flat. The machine uses turning holders that take a 1.25" x 1.0" tool (1" wide, 1.25" high). I am unsure of what insert sizes that means, but I can measure tem with the caliper before I order anything. I have a couple of square holders, and three diamond shaped holders. I heard the diamond shape is more applicable to finsihing AL?

I'll check out Sandvik. I'm guessing you can use any insert in the toolholder right? I mean, they are Kennametal holders but Sandvik inserts would fit provided they are the right size? I am new to turning (mostly milling before) so I apologize for the dumb questions

Cheers!

[Skeeterd5150]

I thought I read in Msc to not use a Tialn Coating. I thought because it had ALuminum as a component of the coating aluminum was more likely to stick to it. I am a beginner to all this stuff so this is more of a question than a comment. Wouldn't Ticn be a better coating? I know it doesn't have as high of a heat resistance.

[tobyaxis]

Originally Posted by SRT Mike I am new to turning (mostly milling before) so I apologize for the dumb questions Cheers!

There is no such thing as a Dumb Question here. We weren't born knowing everything you know.

You need to find out what Tool Holders you already have to select the proper inserts for them.

TiALN can be used according to and Artical in MMS.

[SRT Mike]

Originally Posted by tobyaxis There is no such thing as a Dumb Question here. We weren't born knowing everything you know. You need to find out what Tool Holders you already have to select the proper inserts for them. TiALN can be used according to and Artical in MMS.

Well ok dont mind if I do

The profile I am cutting is as I said a bullet shape. I am doing some facing and boring on the wide end so then I'd like to rough out the bullet shape (which is a decreasing size as it gets closer to the chuck). So at the start of the cut I have plenty of clearance but towards the end of the cut, I will be around 1" into the metal - would I just mount the toolholder so that it sticks out maybe 1.25" from the turret? Seems I'm losing rigidity there.

I know I could cut the bullet shape with the part reversed except that will require another setup (which I may need to do anyway to get a good finish) but I'm asking out of curiosity - you just extend the tools out or are there special long holders or something?

[Geof]

Bullet shape? Something like this?

http://www.cnczone.com/forums/attach...0&d=1185236204

Which was machined and anodized without anything other than washing with soap and water.

[SRT Mike]

Originally Posted by Geof Bullet shape? Something like this? http://www.cnczone.com/forums/attach...0&d=1185236204 Which was machined and anodized without anything other than washing with soap and water.

Geof,

That is almost exactly what I am doing - well, if you take the parting line around the center of the bullet part, and then everything from there over to the right (towards the blue hose). My bullet shape is similarly shaped, has a large opening on one end, tapers to a rounded nose at the other, and has a hole about half way down on the exterior surface.

Do you mind if I ask what material that is? Mine will be 6061 AL. Is it 6061 or another flavor of AL? May I ask what type of toolbits you used to machine that? And also, did you cut the hole in the outside with a 2nd op on a mill or live tooling on the lathe? And did you use 2 setups to cut that or did you core it out and turn the exterior shape in one fixture then just part it off? I think I will need two fixtures, first to cut the internal cavities and the 2nd to rough and finish the bullet shaped exterior.

Looks like a neat little part you got there - is it a phaser or some sort of proctological probe maybe?

[Geof]

Material is 6061 T6.

Picture below shows the tool; diamond with 30 degree tip and .008 nose radius or something like that.

Both parts were finished inside and threaded and roughed on the outside then screwed onto mandrels for the full outside finish. As far as I can remember the final cut was 1800 rpm, around .01" DOC (diameter measure and a feed of .003" per rev., I would need to look at the program to confirm these.

The side hole for the mounting boss was done on a mill.

I should defy you to figure out what it is but I will relent. The mouthpiece on the left gives a little hint but possibly a misleading one. In the jargon of today it is a Human Interface Device aka Mouth Operated Joystick Mouse. It is for people with high level spinal cord injuries who do not have much muscle control below the neck to control a cursor on the PC. Moving the mouthpiece up/down/sideways give full cursor control; puffing into the mouthpiece gives left click, sucking gives right click. All the electronic stuff inside was developed locally by a society for people with disabilities; I am doing the mechanical design and prototyping and financing a start-up company that will manufacture and market it along with some other products for people with a disability.

I am quite proud of it, totally hand coded.

[tobyaxis]

Geof,

You hit the Nail on the Head again Buddy. You are a crafty one, LOL.

[keitholivier]

Not sure if it has been covered already, but a key to getting a good finish is to keep the swarf away from the surface being cut. High pressure coolant can help flush all the stuff away. If you end up re-cutting swarf it makes a mess of everything. Odly enough, this can sometimes be a problem with a very light cut since the swarf is finer and may cling more.
Keith